Re: [Xcircuit-dev] XSPICE output possible?

[Matthew J. <jac...@co...>]

R. Timothy Edwards wrote:
> Dear M.,
>
>> First off, I LOVE this program. I use it for just about everything I 
>> can because of the seamless transition from design / simulation to 
>> publication quality figure insertion.
>
> I don't know how many published circuits I've seen containing drawing
> errors.  Everyone knows that you always use the same source circuit
> file to simulate and do LVS, but there's no such consensus that you
> should always use the same source circuit file to simulate, do LVS,
> AND publish.  It's like they treat it as clip art or something.
This is precisely what brought me to this tool to begin with. I was 
absolutely shocked to discover that very high-dollar, high-profile EDA 
tools (e.g. Cadence, Synopsys, etc.) produced awful graphical output 
without some convoluted, ineffective process. Toss in the fact that you 
can directly insert LaTeX into the schematic and it's a no-brainer. I 
must admit that I didn't initially use XCircuit for schematic capture. 
It was the most viable alternative to Dia, Visio, and Kivio. That being 
said, once I discovered the capability to produce SPICE compatible 
output, I haven't looked back. Again, I offer GREAT THANKS to those that 
have put forth so much effort into this project.
>
>> I am currently trying to use XCircuit to do some mixed-signal 
>> modeling and am having a difficult time generating the proper XSPICE 
>> syntax from the 'spice' line.
>>  
>> For XSPICE, I have to deal with behavioral nodes which are vectorized 
>> [nodes must be in brackets] as shown below:
>>  
>> XSPICE netlist -
>> ainv1 [logic_input] [logic_output] xspice_inverter
>> .model xspice_inverter inv1(blah blah blah)
>>  
>> I have tried every possible permutation imaginable on the %p pin 
>> designation to get the brackets included in the output. If this is 
>> possible, I would be very thankful if someone would show me how.
>
> I take exception to your use of the phrase "every possible permutation",
> since you missed the one that works.  
Dually noted ....
> Anyway, it is helpful to understand
> that the "usual" syntax, e.g., %pin %pout, is really just a shorthand
> notation that relies on there being expected whitespace after the pin
> name in the output file.  In all other cases, the pin name should be
> enclosed in quotes so that xcircuit knows, for example in your case,
> that the pin name is "in" and not "in]".  So, the correct xcircuit line
> is:
>
>     spice:ainv%i [%p"in"] [%p"out"] xspice_inverter
>
> I admit that's a bit subtle.
>
>                     Regards,
>                     Tim
That works like a charm. And it's much more intuitive than my 'work 
around' .... I did the following:

    spice: xinv%i    %plogic_input    %plogic_output    my_inverter
    spice:.INCLUDE /some/directory/here/work_around.mod

    *////////////////////////////////////////////
    * work_around.mod contents:
    *////////////////////////////////////////////
    .subckt   my_inverter   input   output  
    ainv    [input]   [output]   xspice_inverter
    .model xspice_inverter   inv(blah blah blah)
    .ends

Thanks again for the response. The 'correct' procedure is far more 
intuitive than my convoluted work around. Consequently, the capability 
to provide direct XSPICE compatible output allows for XCircuit to 
function as an effective schematic capture front end to a true 
mixed-mode simulation environment (I use ng-spice currently). That is 
nothing short of amazing!

I don't fancy myself as a 'coder', but if ever I could offer a 
contribution of time to this project, please let me know. Thanks again 
for providing such a great tool!

Matthew Jackson
Hardware Design Engineer
JT3 LLC